Revision History

 

Note

All SolidPractices are written as guidelines. It is a strong recommendation to use these documents only after properly evaluating your requirements. Distribution of this document is limited to Dassault Systèmes SolidWorks employees, VARs, and customers that are on active subscription. You may not post this document on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SolidWorks Corporation.

This document was updated using version SOLIDWORKS 2022 SP3.0. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.

Preface

Much of the success of any endeavor owes more to the planning than to the execution. Why would finite element simulation be any different?

When tackling a new simulation challenge, too many engineers hastily give in to the urge to see some results. They run an ill-conceived study that is at best useless, and is often misleading. With better planning, these engineers could avoid disappointment, struggle, and disillusionment.

In practice, there is much to do before creating a study. It starts with determining the scope of the simulation that you plan to run, and knowing what decision you want the simulation results to help you make. With that in mind, you can start the process of creating the suitable geometry that you use as a support for your study. This is an iterative process, during which you must consider compromises when facing mutually exclusive requirements.

As your experience grows, you reap more and more of the benefits of using better modeling and meshing practices.

Your Feedback Requested

We would like to hear your feedback and suggestions for new topics. After reviewing this document, please take a few minutes to fill out a brief survey. Your feedback will help us create the content that directly addresses your challenges.

1. Before You Begin
2. The Planning Stage

Before creating your study, and even before creating your first sketch for that matter, you must anticipate and determine the scope of the simulation that you plan to run.

This scope is multidimensional, and consists of three domains:

• The scope of the phenomena to represent, and the types of numerical results to use for evaluation.
• The scope of the portion of the universe to take into account (the structure of interest + its surrounding environment?)
• The scope of the level of detail required from a geometric standpoint and from a numerical standpoint.

The following illustration describes the procedure well:

Required Level Of Accuracy & The Spiral

This may come as a revelation to you: Results do not have to be valid.

From a practical standpoint:

1. Users seek simulation results to reach a decision.

🡺 Example of decision: Is overheating a concern? Is it stiff enough? Is yielding a concern?

1. Results only need to be as accurate as required for the current decision.

🡺 Depending on the type of decision, and whether you are only running a quick and dirty simulation to validate an alternate design, maybe an approximation is enough!

The level of detail you need in your results depends on the decision you make. If you describe the decision in a broad way, then you do not need very accurate results. As you go further in the design process, the decisions you make become more and more refined. Consequently, your geometry and your expectations about the result accuracy become more refined also.

Therefore, the model you use for your simulations evolves along with your design process and include more details, which lead to progress.

Consider the following visual representation of a spiral. The idea of the spiral came from the North American SOLIDWORKS VAR CAPINC.

Absolute values are irrelevant

Only the trend matters

Initial impression

Doom detection

1st quantitative results

(Hand calculations)

(Lab tests)

Final validation

As realistic as possible

: Gives an initial impression about the design. It helps determine whether some design ideas are promising, or doomed to fail. At this stage, the geometry is not refined. Rough estimates of results are sufficient.

Spiral 2: Absolute values remain of little importance. At this stage, you first review the trends and patterns to select between options. This stage helps you select one design alternative over another. Only then can you start quantifying the results.

Spiral 3: After choosing your design, you must refine the design details. That is, you must determine the thickness and fillet sizes. You now care about the result values.

Everything Starts With the Geometry

In SOLIDWORKS, users typically create geometry with manufacturing in mind, and create their models so that they can generate drawings and bills of material later. The models also typically only use solid geometry, and they include all components including pins, bolts, and washers. They also include gaps for ease of assembly and sometimes include cuts at the interface between parts for weld beads.

All the requirements of manufacturing are usually present in a SOLIDWORKS model.

However, users generally ignore the simulation requirements. These requirements include for example:

• A meshable geometry
• A model small enough to run in an acceptable amount of time
• Geometry items to apply loads fixtures, connections
• Management of contacts

All the requirements of manufacturing are often a burden for simulation.

In addition, not all of the manufacturing requirements are relevant to simulation.

Therefore, for simulation, why would you use a model that is designed with manufacturing in mind?

1. Decide on the area of interest in the model. Determine the components in which you want to determine stress and displacements under the given conditions.
2. Remove all components that do not participate in the simulation because:

• They bear no load.
• They are replaceable in the model by their effect on the areas of interest (replace by a load, a boundary condition, or a connector).
• You purchase these components and therefore only load levels are important in them, not stress. You select the components based on the supplier's allowable loads. You can replace them with connectors.

1. Among the remaining components, assume use of a solid mesh for all of them. Then, study each component one after the other. Imagine if each component was treated as a shell, and ask yourself:

• Would a surface representation be truthful to the geometry (not the case for bulky parts for example)?
• Would a surface representation achieve sufficient accuracy for the interaction with other parts and with the application of loads, fixtures, and connectors?
• Would it be too much work to convert the solid geometry to surface when compared to the benefit (decrease of memory requirements and computational time)?

1. Ask the same thing about beam elements, while fully understanding the consequences of beam modeling (extreme simplification of geometry, different types of stress outputs, connection with other components).

Each time you decide to change the type of elements used for a component, this has consequences on the geometry required for meshing that component. There are also consequences on the geometry required for meshing the other connected components because connections must be truthful to reality. Therefore, it is an iterative process where each decision can invalidate other decisions and eventually, you have to find a compromise.

• Versions 2021 and 2022 include many changes and improvements in the way that interactions work. Be sure to familiarize yourself with this topic.

Solid Modeling Guidelines For Solid Meshing

The following guidelines are helpful to troubleshoot geometry-related meshing problems when you want to have a solid mesh.

• Whenever you are using imported geometry (Parasolid, ACIS, IGES and others):
  • Run the Import Diagnostics tool. This tool can detect faulty faces. Heal all the faces.
  • Consider using the FeatureWorks® automatic feature recognition software to have SOLIDWORKS build a FeatureManager® tree. This makes adjustments to the geometry easier, and it might make meshing easier.

• Use the tools in the Analysis Preparation CommandManager toolbar to conform the geometry to your meshing and simulation requirements. Particularly useful tools include Simplify, Combine, and Split. You can also access the Simplify tool if you right-click Mesh and select Simplify Model for Meshing.
   

  
• Use the SOLIDWORKS Check option to review your model for geometry errors. To access this option, go to Tools > Evaluate > Check. This option helps reveal non-valid faces and edges. You can also use the Geometry Analysis tool, which is more powerful. See Appendix A – Using The Geometry Analysis Function to Check The Geometry.

•  

  , a model needs the minimum number of cosmetic features. If there are any features that you think do not contribute to or affect the results, then it is a good practice to suppress those features before you mesh the model.

   

• When dealing with assemblies or multibody parts, use the Interference Detection tool (Tools > Evaluate > Interference Detection) to detect any unwanted interference in the model. Interference is expected if a shrink fit condition exists. In other cases, it is better to remove interferences. Be aware that you can still bond components that have a slight interference if you are using an independent mesh.
• For hard to mesh parts, you might want to split the part into pieces. Try to create individual pieces that are easier to mesh as the following image depicts. Make sure that you can mesh the pieces by trying to mesh each one of them separately.

Preparing A Solid Model For Mixed Meshing

After determining that the mixed meshing method is appropriate for the analysis of a model, perhaps the most important step of the analysis process is to prepare the model for meshing. Ninety-nine percent of the time, you begin with a full solid model. Therefore, you must convert some of the solid parts to surfaces. Depending on the complexity of the model and how the model is built (with few complex parts, or with several simple parts in an assembly), make a decision about whether you want to create the surface parts from scratch, or work from the existing solid geometry. Recreating the surface parts from scratch is a good idea if the existing solid parts are too difficult to work with. It is interesting to work from the existing solid geometry to maintain the associativity between the surface model and the solid model.

Follow these steps to create the surface geometry from the solid geometry:

1. Create a new configuration. Call it Surface Geometry for example.
2. From the existing solid geometry, use the Midsurface and Surface Offset features to create the midsurface. This represents the solid geometry. Finalize the surface or mixed geometry using Extend, Trim, and Untrim features, and possibly other features.
3. Suppress the solid bodies in the Surface Geometry configuration you created.

Example Of A Simple Part

First, consider a simple plate that you obtain by using an Extrude feature. Be aware that the plate thickness in the following figures is enlarged for visibility.

Figure 1 depicts the original solid model.

Figure 2 depicts the surface model in the Surface Geometry configuration. The MidSurface feature was used to create the surface. The solid body was then deleted in this configuration.

Figure 3 depicts the modified solid model in the Default configuration. In this configuration, the MidSurface and Body-Delete features are suppressed to keep the original solid geometry in this configuration.

The advantage of creating the surface geometry using the method shown in Figure 3 is that changes to the dimensions of the solid model automatically update the dimensions in the surface model.

Example Of A More Complex Part

Now, consider a more complex part. The part in Figure 4 consists of a combination of welded thin plates, hinges, and locks. This particular model has half hinges and locks.

Here, you need to model the plates using surfaces, and keep the more bulky areas of the model as solid bodies.

The first step again, is to create a surface geometry configuration.

Then, you must edit the features used to create the hinges and the locks so that you can deactivate the Merge Result option to create separate solid bodies. Then convert all of the plates to surfaces using the MidSurface feature for each of them.

After creating all of the midsurfaces, you can use the Extend, Trim, and Untrim features, and possibly other features to adjust the midsurfaces together (see Figure 5). Use these features wherever the MidSurface feature creates surfaces that either:

• Have a gap while they should touch
• Overlap or intersect when they should have a common edge instead

Finally, when the surface model is complete, you can use the Delete Body feature to suppress all of the replaced solid bodies with their equivalent surface geometry.

When complete, the model contains six solid bodies (shown in green highlight in Figure 6), and many surfaces that represent the thin plates.

1. Full assembly model

You can then integrate all of the parts into the assembly, or in a new configuration.

1. Defining the interactions in the study

This is another crucial step. The following SOLIDWORKS Knowledge Base solutions discuss this topic and are a useful source of information:

• Solution ID: S-019615 - What are the differences between Surface to surface, Node to surface and Node to node contact elements?
• Solution ID: S-018846 - Recommendations on creating local Contact interactions
• Solution ID: S-018871 - How do I use bonded interactions using constraint equations?

In addition, the Online Help provides the most up-to-date information about the capabilities of the SOLIDWORKS version you are using. In particular, read these help topics:

• Guidelines on Studies with Interaction Conditions
• Automatic Bonding Between Touching Entities
• Component Interaction PropertyManager
• Local Interactions PropertyManager
• Interaction Viewer PropertyManager

If you construct your geometry correctly, it is simple to create the interactions and you do not need to create too many of them. You can use the Local, Component, or Global types of interactions to define a bonded interaction condition. You might have to create a number of contact interactions, depending on the complexity of the model. For larger models, it is always more efficient to rework the geometry to avoid having to create too many contact interactions.

Important final recommendations:

• Avoid creating interactions automatically. This typically generates an overly large number of interactions. Also, the automatic algorithm is unable to group the geometric entities in these interactions in the same efficient way that an experienced user would. It is better to use your engineering judgment and define the interactions manually.
• Before you run the study, use these diagnostic tools. They can help reveal shortcomings in the setup of the study.
  • Always use the Interaction Viewer PropertyManager to review the solver-based interactions. This review may help you determine if you need to make some adjustments to the interactions.
  • Use the Underconstrained Bodies tool to identify bodies with underconstrained degrees of freedom. This is particularly helpful for models with a large number of bodies.

1. Surface Geometry Creation Example: From Solid To Meshable Surface Geometry
2. Scope

For the example in Figure 8, the scoop was modeled in solids initially for styling purposes. However, the problem embodies several complex nonlinearities. Therefore, a simpler, faster idealization is important to assess the stiffness and to place the ribs optimally. There could be 10-12 iterations in pursuit of the final design, so it is important to shave as much time off the solution as possible.

After making the decision to analyze this part as a shell mesh, you need to investigate ways to convert the model to a surface representation. Simply choosing the outside or inside surfaces is not an option in this problem for two reasons:

• The first reason is that the t-joint nature of the handle to scoop interface places a wall with thickness on the back of the scoop:
  • If you selected the outer surface of the scoop to generate the surface body, the resulting geometry would have slot-like cut-outs where the wall of the handle intersected. Therefore, this would not be a good choice.
  • If you selected the inner surface of the scoop to generate the surface body, the resulting geometry would have two bodies separated with a gap. You could still define a bonded interaction between free edges of the handle and the scoop. This is a good choice in SOLIDWORKS 2021 or more recent because of enhancements to bonded interactions. It is relatively easy to obtain a geometry without gaps. This is what the procedure shows.
• The second reason is that the features of the handle are not significantly larger than the wall thickness. Approximating the geometry by using either the outer face or the inner face of the solid model introduces errors that are not negligible when the wall thickness approaches the size of the feature. Using the Shell offset option during the shell definition is not sufficient to resolve these problems. Therefore, it becomes even more important to use mid-surfaces to obtain a proper geometric representation. Mid-surfaces are required.

Therefore, the task is to create a surface model out of the solid model. The surface model should accurately represent the mid surfaces of the solid model. Also, in the present case, make sure to create the surface model to ensure a compatible mesh. This is not an absolute requirement because it is possible to define a bonded interaction between entities that a small gap separates.

1. Step-by-step procedure
2. Create surfaces that are offset by ½ thickness from the inner or outer faces of the handle (your choice). Figure 9 depicts use of the inner faces.

The Insert > Surface > Midsurface feature did not work for this model because the model is too complex for the automated tool to resolve. However, the Insert > Surface > Offset feature works fine. Using the Select Tangency option, all of the handle surfaces are offset into the part by ½ of the wall thickness.

1. Do the same thing for the faces of the scoop.
2. Suppress the solid body. Use the Insert > Features > Delete Body feature.

Notes:

• After creating the surfaces, the solid body was no longer of any use. Therefore, it is ok to delete the solid body from the Solid Bodies folder. This results in a feature in the tree with the name Body-Delete1. You can delete or suppress this feature later if you want to bring the solid back. Removing the solid from the model allows you to examine the surfaces.
• Unfortunately, this results in a ½-wall thickness gap between the handle surfaces and the scoop surfaces. These need to be joined by using the surfacing techniques in the SOLIDWORKS application. You have the option to extend existing surfaces, however the end condition of the handle is complex for this technique. Therefore, consider trimming the complex ends back to a properly positioned plane by using the Insert > Surface > Trim feature. It is then easy to extend the squared off edges through the scoop, and then to make adjustments using a Trim function.

1. Create a plane in the location shown in Figure 11 (Plane3) and then use the Insert > Surface > Trim feature to nicely cut the surfaces.

1. Next, use the Insert > Surface > Extend feature to extend the newly cut surfaces so that they intersect the surfaces of the scoop.

1. You can now trim the extended faces to adjust them to the shape of the surfaces of the scoop. Once again, use the Insert > Surface > Trim feature.

1. Finally, create a closed sketch using the edges of the recently trimmed surfaces so that you can split the surfaces of the scoop along the same lines. Use the Insert > Curve > Split Line feature.

Creating this split line ensures that touching faces share common edges. This way, the mesher can create a compatible mesh. If you want to skip this step you can, however you must then manage the bonding by creating a Bonded type of interaction between the edges of the handle and the faces of the scoop. 

Examples Of When Not To Use Beams

Although the SOLIDWORKS Simulation software automatically treats all of the structural members in your model as beams*, this does not mean that you must always accept this default setting. Using beam elements to represent a solid geometry has major consequences on the representation of the structure, the mesh, the results, extreme simplification of geometry, different types of stress outputs, and connections with other components. Do not let the software choose the appropriate type of element to use to represent a body! Only humans have the engineering sense to do this.

* Starting with version 2021, you can change this default behavior. To do this, activate Simulation > Options > Default Options > Mesh > Mesh all solid bodies with solid mesh. With the option active, SOLIDWORKS Simulation meshes all solid, sheet metal, and weldment bodies with a solid mesh. At a study level, you can override the mesh assignments that this option specifies. In a simulation study tree, right-click the top Parts folder, and select Treat all sheet metals as shells or Treat all weldments as beams.

The presence of cutouts, holes, or geometry irregularities along the length of beams has a negative impact on the beam analysis results and also on the 3D rendering of the beam mesh and results plots. The recommendation is to remove any cutouts, holes, or geometry irregularities from the structural members, before you create the beam mesh and run the analysis. If you cannot remove any geometry irregularities present along the length of structural members, use a solid mesh instead of a beam mesh for more accurate results.

There are many more consequences to treating a body as a beam or as a solid. The following table lists the main consequences:

The following examples depict cases where beam elements are not the preferred type for various reasons:

1. Example 1

In Figure 15, the vertical I beam should not be treated as a beam if it is important to consider the triangular stiffeners.

Effective with the release of SOLIDWORKS Simulation 2013, the software supports the bonding of a shell edge and a beam (gusset). However, with beam modeling, it is not possible to attain the level of detail of the design shown in the image.

1. Example 2

In Figure 16, the horizontal U beams should not be treated as a beam because it would then be impossible to represent the connection with the pin.

1. Example 3

In Figure 17, the I-beam should not be treated as a beam if it is important to consider either the superimposed rectangular flat plate or the other stiffener.

1. Example 4

In Figure 18, the I-beam should not be treated as a beam. A beam mesh cannot accurately represent the bonded connection of the plate onto the flange of the I-beam.

1. Example 5

In Figure 19, the larger blue beam should not be treated as a beam. Under this loading condition, the blue beam experiences some bending, torsion and shear. A beam mesh is able represent the associated deflection. Another, more significant source of deflection is the change of shape of the cross section, going from square to rhombus. Only a shell or solid mesh are able to take this deformation into account.

Here is a comparison of the resultant displacement result plots using a beam mesh (left) and a solid mesh (right), at the same deformation scale. Notice the deformed shape of the cross section of the larger beam with the solid mesh.

Meshing Strategy

Many consider meshing to be a form of art. A talent that comes after years of painstaking experience.

This is not so true anymore as modern software automate most of the mesh creation. Each software has its own peculiarities however, and you cannot expect to successfully mesh difficult models before you have explored and understood the specific tools and options at your disposal in your software.

It is therefore important to read the documentation. It is even more important to practice.

Examples of relevant Help topics:

• Meshing Options
• Meshing Tips
• Mesh Control Examples
• Mesh Failure Diagnostics

In SOLIDWORKS Simulation, users rely on some of the following strategies to help with meshing when they encounter difficulties:

Checking the quality of the mesh

After meshing, review the quality of the mesh using the Mesh quality checks and Mesh Quality Diagnostic tools.

The absence of distorted elements and high aspect ratio elements in your mesh is not sufficient to ascertain that the mesh is well suited to fully capture the physics of the simulation.

In static studies, plotting the ERR: Energy Norm Error result helps determine the discretization error from insufficient mesh density. See the Discretization Error Estimation help topic.

Results usually converge to a solution when you rerun the same study with an increasingly refined mesh. This convergence is essential in determining that your mesh is well suited for the simulation.

In some cases, at certain locations in your model, the result may instead diverge when you rerun the same study with an increasingly refined mesh. This is usually indicates the presence of a singularity; a location where the stresses are in theory infinite. A typical example is a sharp re-entrant corner in the geometry.

You can use the Stress Hot Spot diagnostics tool to detect regions of the model where stress gradients between adjacent elements are irregular. In certain cases, these irregular high stress gradients can be attributed to stress singularities. However, not all stress hot spots are associated with stress singularities. Refining locally the mesh at hot spot regions can eliminate these stress hot spots attributed to stress concentrations that are nonsingular. See the Assessing Stress Hot Spots help topic.

Appendix A – Using the Geometry Analysis Function to Check the Geometry

SOLIDWORKS has a very good tool to check a model's geometry for small features such as short edges, narrow faces, small faces, and sharp corners that can cause meshing to fail. This function is called Geometry Analysis and is in the Tools > Evaluate menu item.

The Geometry Analysis function is only available for part models.

Geometry Analysis Parameters

You can access Help to understand all of the available options by clicking the

Generally, it is best to use the same length value for all three Insignificant geometry parameters. To determine what value to specify, measure the shortest significant edge on your model. For some models, the shortest significant edge is the plate thickness, or a chamfer, or a hole diameter, etc. Divide this value by 2, and enter that value for the Short edges, Small faces, and Sliver faces length. The Geometry Analysis function automatically detects all insignificant geometry based on the threshold value that you specify.

For Sharp angles, the default value of 5.0deg is usually acceptable.

Geometry Analysis: Results

The Geometry Analysis function returns all detected insignificant geometric features classified by type.

Make it a point to review all detected items. These items often show geometric modeling problems. In particular, the detected short edges and sliver faces can lead to the presence of bad quality elements with a very large aspect ratio. These items might also have distorted elements with a high or negative Jacobian ratio. They can even cause mesh failure.

Useful SOLIDWORKS features to reduce the number of short edges and sliver faces include Insert > Face > Delete (with either the Delete and Patch or the Delete and fill option), and Insert > Face > Heal Edges.

The Standard mesher is capable of merging nodes that are closer than the value you define for Tolerance in the Mesh PropertyManager. If you cannot fix some of the detected short edges and sliver faces, a possible meshing strategy is to write down their size, and use a slightly larger tolerance for meshing. The standard mesher merges the nodes at these locations, and the meshing proceeds properly. This works better for the remaining sliver faces, small faces, and short edges, than for the remaining knife vertices or knife edges.

When selecting the best mesher for your model, evaluate this advantage of the Standard mesher with the advantages of the curvature-based meshers that the Standard mesher does not have. It is a good practice to try all available meshers and to select the mesher that produces the most satisfactory mesh.

We hope that you find this document informational and useful and request that you leave a brief feedback about the topics that you want us to cover in the next revision of this document. Click here for a complete list of SolidPractices documents available from DS SOLIDWORKS Corp.